3.2.31 Translating Abaqus files to Nastran bulk data files
Products: Abaqus/Standard Abaqus/Explicit
References
Overview
The translator from Abaqus to Nastran converts certain entities in an Abaqus file into equivalent entities in Nastran. Only “flat” Abaqus files can be translated; i.e., the Abaqus file cannot contain parts and assemblies.
Using the translator
The Abaqus input data must be in a file with the extension .inp or .sim. If you specify an .inp file, the execution procedure translates selected keywords and creates a Nastran bulk data file with the extension .bdf. If you use the substructure option and specify a substructure .sim file, the execution procedure translates the substructure data to Nastran DMIG coefficients and creates a Nastran bulk data file with the extension .bdf.
Summary of Abaqus keywords translated
In the *ELEMENT usages listed below, an italicized x indicates that all Abaqus elements beginning with the preceding label will be mapped to the Nastran entity shown. For example, the statement *ELEMENT, C3D4x indicates that the selected Abaqus-to-Nastran translation applies to the Abaqus elements C3D4, C3D4H, and C3D4T.
Table 3.2.31–1 Abaqus keyword–to–Nastran mapping.
| Abaqus Keyword | Nastran Complement |
|---|---|
| *BEAM GENERAL SECTION, SECTION=GENERAL | PBAR |
| *BOUNDARY | SPC |
| *CLOAD | FORCE |
| *COUPLING, DISTRIBUTING | RBE3 |
| *COUPLING, KINEMATIC | RBE2 |
| *ELEMENT, B31 | CBAR (for *BEAM GENERAL SECTION, SECTION=GENERAL) |
| *ELEMENT, B33 | CBAR (for *BEAM GENERAL SECTION, SECTION=GENERAL) |
| *ELEMENT, C3D4x | CTETRA |
| *ELEMENT, C3D10x | CTETRA |
| *ELEMENT, C3D6x | CPENTA |
| *ELEMENT, C3D15x | CPENTA |
| *ELEMENT, C3D8x | CHEXA |
| *ELEMENT, C3D20x | CHEXA |
| *ELEMENT, MASS | CONM2 |
| *ELEMENT, ROTARYI | CONM2 |
| *ELEMENT, S3x | CTRIA3 |
| *ELEMENT, S4x | CQUAD4 |
| *ELEMENT, S8x | CQUAD8 |
| *ELEMENT, SPRING1 or SPRING2 | CELAS |
| *ELEMENT, SPRINGA | CROD |
| *ELEMENT, STRI65 | CTRIA6 |
| *ELEMENT, T3D2 | CROD |
| *FREQUENCY | SOL 103 |
| *HEADING | TITLE |
| *MATERIAL, DENSITY | MAT1 |
| *MATERIAL, ELASTIC, TYPE=ISO | MAT1 |
| *MATERIAL, ELASTIC, TYPE=LAMINA | MAT8 |
| *MATERIAL, EXPANSION, TYPE=ISO | MAT1 |
| *MATERIAL, EXPANSION, TYPE=ORTHO | MAT8 |
| *NODE | GRID |
| *ORIENTATION, DEFINITION=COORDINATES | CORD2R, CORD2C, or CORD2S |
| *SHELL GENERAL SECTION (Non-composite) | PSHELL |
| *SHELL SECTION (Non-composite) | |
| *SHELL SECTION (Composite) | PCOMP |
| *SHELL GENERAL SECTION (Composite) | |
| *SOLID SECTION | PSOLID |
| *SOLID SECTION (Trusses) | PROD |
| *STATIC | SOL 101 |
| *SYSTEM | CORD2R, CORD2C, or CORD2S |
| *TRANSFORM |
Command line options
This option is used to specify the name of the Nastran bulk data file to be output by the translator. It is also the default name of the Abaqus file. Diagnostics created by the translator are written to a file named job-name.log.
This option is used to specify the name of the file containing the Abaqus data if it is different from job-name.
This option is used to translate a substructure within an Abaqus .sim file into Nastran bulk data file (.bdf) format.
This option is used to determine how structural damping terms are represented. If complex=YES (default), structural damping terms are written as the imaginary part of the stiffness matrix; if complex=NO, structural damping terms are written as a separate real matrix.